Exercício de Treliça 3d Livro

258 Chapter 7 Line Models Section 7.2 Step-by-Step: 3D Truss 7.2-1 About the 3D Truss Traditionally, a truss is defined as a structure consisting of two-force members. By two-force member, we mean that the members are pin-jointed at the ends and the loads apply on the joints so that the members are either stretched or compressed but not bent. Two members connected by a pin-joint can rotate about the joint independently. In reality, structural members are rarely connected each other by pin-joints. Modern structures are constructed using either welds or multiple bolt-and-nuts; the members are rigid joined, not pin-jointed. Even in the old days, pin-jointed structures are not common. Main reason of pin-joint assumption is to ease the computational difficulty, in the days when computers were not widespread, if existing. Note that, due to the neglect of joint rigidity, pin-joint assumption leads to a conservative design: safer, but over-designed. How much is the error caused by the pin-joint assumption? This is a good exercise problem for the engineering students (Section 7.4.2). Let me state the problem more precisely. Given a rigid-jointed structure, we perform twice of simulations: once with rigid joints (the reality), and the other with pin-joints assumption. What would the difference between these two models be? The amount of error depends on the slenderness of the structural member. If the members are slender enough, there is no essential difference between two models. On the other hand, if the members are not slender enough, then the pin-joints assumption may induce substantial errors. Currently, the beam element (BEAM188) is the only element supported in <Mechanical> to mesh the line bodies. The “truss elements” (such as LINK180) are not directly supported. To model a pin-jointed structure, you need to explicitly specify revolute joints between the structural members, or insert APDL commands. In this section, we will create a line model for the power transmission tower as shown. All members are made of structural steel angle of 1 ½ x 1½ x ¼ cross section. Note that each joint (P1-P10) or member (1-25) is assigned a number. The design loads are also show below. Design Loads for the Transmission Tower Joint Fx (lb) FY (lb) Fz (lb) P1 1,000 -10,000 -10,000 P2 0 -10,000 -10,000 P3 500 0 0 P6 600 0 0 Section 7.2 Step-by-Step: 3D Truss 259 PART A. GEOMETRIC MODELING 7.2-2 Start Up (1) Launch <Workbench> and save the project as “Truss.” (2) Create a <Static Structural> system. (3) Start up <DesignModeler>, Select <inch> as length unit. 7.2-3 Create 10 Construction Points in the 3D Space 1 1 -37.5 0 200 2 1 37.5 0 200 3 1 -37.5 37.5 100 4 1 37.5 37.5 100 5 1 37.5 -37.5 100 6 1 -37.5 -37.5 100 7 1 -100 100 0 8 1 100 100 0 9 1 100 -100 0 10 1 -100 -100 0 (1) Prepare a TEXT FILE containing coordinates of 10 points, and save it in your disk. Note that the file has 5 columns (fields): (a) group number, (b) ID number, (c) X-coordinate, (d) Y-coordinate, and (e) Z-coordinate. The group number and ID number are arbitrary, and they uniquely identify a point from others. Numbers can be separated by spaces or TABs. Point O (2) Click <Point> on the toolbar. (3) Select the TEXT FILE. (4) Click <Generate> (5) The points show up in the graphics space. Note that the model has been rotated such that XY plane lies horizontally. Details of Point Point Point1 Type Construction Point Definition From Coordinates File Coordinates File TEXT FILE Tolerance Normal Refesh No 276 Chapter 7 Line Models Point X Coordinate Y Coordinate Z Coordinate (in) (in) (in) 1 -37.5 0 200 2 37.5 0 200 3 -37.5 37.5 100 4 37.5 37.5 100 5 37.5 -37.5 100 6 -37.5 -37.5 100 7 -100 100 0 8 100 100 0 9 100 -100 0 10 -100 -100 0 [5] Repeat steps [1-4] for additional nine points (Points 2-10). Their respective coordinates are tabulated here. [6] Newly created points. (The numbers are added by the author for reference.) Note that the model has been rotated such that Z-axis directs upward. Using <Coordinates File> to Define Points An alternative way of defining points is to select <From Coordinates File> for <Definition> and read the coordinates from a file [7,8]. When the number of points is large, this is obviously a better way to input coordinates. A <Coordinates file> [8] is a text file describing the coordinates of points. The file has 5 columns, or fields: (a) group number, (b) ID number, (c) X-coordinate, (d) Y-coordinate, and (e) Z-coordinate. The group number and the ID number can be arbitrarily chosen and they together uniquely identify a point from others. Fields of numbers can be separated by spaces or TABs. You may prepare the text file using a text editor; another way is using a spread-sheet program such as Microsoft Excel and saving as a text file. Details Var Details of Point Point Point1 Type Construction Point Definition From Coordinates File Coordinates File None Tolerance Normal Refresh Yes [7] An alternative way of defining coordinates is to select <From Coordinates File> for <Definition> and read the coordinates from a file. [8] The format of a coordinate file. 1 1 -37.5 0 200 2 1 37.5 0 200 3 1 -37.5 37.5 100 4 1 37.5 37.5 100 5 1 37.5 -37.5 100 6 1 -37.5 -37.5 100 7 1 -100 100 0 8 1 100 100 0 9 1 100 -100 0 10 1 -100 -100 0 7.2-4 Create a Line Body for 19 Members [1] Pull-down- select <Concept/Lines From Points>. [3] Click <Generate> [4] A line body of 19 members is created. Note that the members do not cross over each other. That is the reason we left out 6 members. [2] Define all members except 3, 5, 15, 17, 19, and 21 (Section 7.2-1), and then click <Apply>. Each member is defined by clicking its starting point then control-clicking its ending point. If you made a mistake, you can remove a member by clicking its starting and ending points again. 7.2-5 Create Another Line Body for the Rest of Members [1] Pull-down- select <Concept/Lines From Points>. [4] Click <Generate> [5] A line body of 6 members is created. [2] Define the rest of members (6 of them) and click <Apply>. [3] Select <Add Frozen> to avoid adding the materials together, i.e., crossing over each other. 7.2-6 Form a Single Part [1] So far we have two parts in the model tree. We now combine them to form a single part. [3] Now we have a single part of two bodies. [2] Select the two bodies and right-click-select <From New Part>. 7.2-7 Create a Cross Section [1] Pull-down-select <Concept/Cross Section/L Section>. [2] Type dimensions for the steel angle. 7.2-8 Assign the Cross Section to the Line Bodies [1] Select two line bodies. [2] Select the cross section <L1>. 7.2-9 Check the Sections in the Model [1] Turn on <View/ Cross Section Solid>. Turn off <Cross Section Alignments> if it is on. [2] The cross section has been correctly assigned to the line bodies. [4] The default cross section alignments are shown. [3] Turn on <View/Cross Section Alignments>. [5] Close DesignModeler. [1] Right-click <Geometry> and select <Properties>. [2] Turn on <Line Bodies>. Without turning it on, the line bodies would be ignored and not attached to <Mechanical>. Close the <Properties>. [3] Double-click <Model> to start up <Mechanical>. Section 7.2 Step-by-Step: 3D Truss 263 The default cross section alignments usually need to be adjusted to be consistent with the reality. In this case, we decided to leave them as default. Since the structural members are slender enough, the behaviors are close to two-force members, therefore alignments should not be critical. In other words, cross section alignments do not affect the structural response too much in this case. We will demonstrate the adjustment of cross section alignments in Section 7.3-9, in which the alignments must be adjusted, or it would deviate the reality too much. PART B. SIMULATION 7.2-10 Set Up Properties for Geometry 280 Chapter 7 Line Models PART B. SIMULATION 7.2-7 Start Up <Mechanical> [2] Close <DesignModeler> and double-click <Model> to start up <Mechanical>. [3] Select in-lb-s unit system. 7.2-8 Generate Mesh [1] Highlight <Mesh>. [2] Type a large number (say 999 in) for <Element Size> to ensure each member is meshed with a single beam element. Select <Mesh/ Generate Mesh>. [3] Totally 37 beam elements (one element for each line segment) generated. Note each beam element has a mid-node on it, so totally 53 (16+37) nodes. Why mesh each member with single element? We mentioned (7.1-16) that it is possible to obtain a solution equal to theoretical values by meshing each straight beam with a single element. The reason we meshed each member with a single beam element here is to demonstrate this. The default settings of <Mesh> would mesh the model with 205 beam elements and would result exactly the same solution as 37 elements. As an exercise (Section 7.4-2), verify it yourself after the completion of this section. Using Surface/Line Models Whenever Possible Since the solution of a model which is meshed with beam elements or shell elements converges very fast (i.e., very accurate solution can be obtained with only a few elements), we should consider a line model or surface model whenever possible. This is particularly true for those problems requiring many number of iterations or substeps, such as nonlinear problems, dynamic problems, optimization problems, etc. 264 Chapter 7 Line Models 7.2-11 Generate Mesh [1] Highlight <Mesh>. [2] Select <in-lb-s> unit system. Type a large number (say 999 in) for <Element Size> to ensure each member is meshed with a single beam element. [3] Select <Mesh/ Generate Mesh>. [4] Totally 25 beam elements (one element for each member). Note each beam element has a mid- node on it, so totally 35 (10+25) nodes. [5] They look like bonded together, but actually not. Each member corresponds to an element. Why mesh each member with a single element? We mentioned in the end of last section (7.1-17) that it is possible to obtain a solution equal to theoretical values by meshing each straight beam a single element. The reason we meshed each member with a single beam element here is to demonstrate this behavior. The default settings of <Mesh> would mesh the model with 205 beam elements and would result exactly the same solution as 25 elements. As an exercise (Section 7.4-2), verify it yourself after the completion of this section. Using Surface/Line Models Whenever Possible Since the solution of a model which is meshed with beam elements or shell elements converges very fast (i.e., very accurate solution can be obtained with only a few elements), we should consider a line model or surface model whenever possible. This is particularly true for those problems requiring many number of iterations or substeps, such as nonlinear problems, dynamic problems, optimization problems, etc. Section 7.2 Step-by-Step: 3D Truss 265 7.2-12 Specify Supports [1] Highlight <Static Structural> in the project tree and select <Supports/ Fixed Support>. [2] Select 4 vertices at the base. You may need to turn on vertex select filter. [3] And click <Apply>. 7.2-13 Specify Loads [1, 3, 5, 7] Select <Loads/Force>. [2] Select P1 and click <Apply>. Make sure the triad is as shown, so that you don’t select the wrong point. [4] Select P2 and click <Apply>. [6] Select P3 and click <Apply>. [8] Select P6 and click <Apply>.